Hey Nick,
you did not say anything about machine model, CNC controller, firmware version, involved accessories.
Setting an offset can be done by probing, e.g. with the XYZ Touch plate. After the probing, you will see that the coordinates have changed (the three columns “Position”, “Absolute” and “Offset” on the CONTROL page).
After probing, the zero coordinate of the coordinate system in effect is now no more at home position, but at the workpiece zero coordinate.
If you want to set the offset manually, it is the G92 – Coordinate System Offset command that sets it if you enter it in the manual data interface (MDI).
The G92 – Coordinate System Offset command is also the most important command in every ‘tool-change’ routine on the SETTINGS page as it sets the Z offset for the new bit length after a bit change.
So after probing, if you use G0 (rapid move) to move to a specific coordinate, like:
G0 X0 Y0
, it will not move to the home position, but to the workpiece zero that you previously probed with the touch plate.
If you nonetheless would want to move in machine coordinates instead of workpiece coordinates then, the you’ll have to prepend G53 – Move in Machine Coordinates, like this:
G53 G0 X0 Y0
This will not alter the offset you probed previously, it will only interpret the X0 Y0 as absolute machine coordinates.
Note that the “Position”, “Absolute” and “Offset” columns on CONTROL page reflect the machine coordinate position (“Absolute”) and the offset (“Offset”). The “Position” column tells the position with respect to your workpiece zero coordinate.
You can also click the “zeroing” buttons on the CONTROL page that will set the offset workpiece zero coordinate by simply clicking on it, either for an indivdual axis, or for all X, Y, and Z axis at the same time:
Image: The “zeroing” buttons on CONTROL page
If you want to know everything about the different coordinate systems that you can use, you can follow this link:
There, you can also learn to know that you can also program multiple offsets at the same time with G54-G59.3 Select Coordinate System so that you can quickly switch between them (manually or from the inside of a g-code program)
You also learn that a tool table is done by programming offsets.
I think you’ll learn g-code if you simply try things out into the manual data interface (MDI), otherwise it’s like you use a CNC machine but sitting only on co-driver seat all the time.